FANUC Series 30i-MODEL B, 31i-MODEL B, 32i-MODEL B. For Machining Center System. OPERATOR'S MANUAL

6.COMPENSATION FUNCTION

PROGRAMMING

B-64484EN-2/02

Post-compensation path

Re-calculation

Programmed path

Block 1

Block 8

Block 1

Block 8

Post-compensati

Post-compensation

on intersection

Post-compensation

vector between

intersection vector

intersection between

block 1 and

between block 1

gap vector and block 8

block 8

and gap vector

Block 2

Gap vector

Block 7

Block 2

Block 7

Block 3

Block 6

Block 4

Block 5

In this case, the post-compensation end points of blocks 2 to 7

coincide with the end point of block 1. Thus, after compensation,

blocks 2 to 7 will be blocks without tool movement.

Fig. 6.6.6.3 (b)

If the tool radius/tool nose radius compensation value is greater than the radius of the specified arc as

shown in the Fig. 6.6.6.3 (c), and a command is specified which results in compensation with respect to

the inside of the arc, interference is avoided by performing intersection calculation with an arc command

being assumed a linear one. In this case, avoided vectors are connected with linear interpolation.

Post-compensation path

Programmed path

Fig. 6.6.6.3 (c)

- 232 -

B-64484EN-2/02

PROGRAMMING

6.COMPENSATION FUNCTION

If no interference avoidance vector exists

If the parallel pocket shown in the Fig. 6.6.6.3 (d) is to be machined, the end-point vector of block 1 and

the end-point vector of block 2 are judged to interfere, and an attempt is made to calculate, as an

interference avoidance vector, the intersection vector of the post-compensation path of block 1 and the

post-compensation path of block 3. In this case, because blocks 1 and 3 are parallel to each other, no

intersection exists. In this case, an alarm will occur immediately before block 1 and the tool will stop.

Stopped

Tool center path

Programmed path

Block 1

Block 3

Block 2

Fig. 6.6.6.3 (d)

If the circular pocket shown in the Fig. 6.6.6.3 (e) is to be machined, the end-point vector of block 1 and

the end-point vector of block 2 are judged to interfere, and an attempt is made to calculate, as an

interference avoidance vector, the intersection vector of the post-compensation path of block 1 and the

post-compensation path of block

3. In this case, because blocks

1 and

3 are circular, no

post-compensation intersection exists. In this case, an alarm will occur immediately before block 1 and

the tool will stop, as in the previous example.

Programmed path

Tool center path

Stopped

Block 1

Block 3

Block 2

Fig. 6.6.6.3 (e)

- 233 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64484EN-2/02

If it is judged dangerous to avoid interference

If the acute-angle pocket shown in the Fig. 6.6.6.3 (f) is to be machined, the end-point vector of block 1

and the end-point vector of block 2 are judged to interfere, and an attempt is made to calculate, as an

interference avoidance vector, the intersection vector of the post-compensation path of block 1 and the

post-compensation path of block 3. In this case, the movement direction of the post-avoidance path

extremely differs from the previously specified direction. If the post-avoidance path extremely differs

from that of the original command (90° or greater or 270° or less), interference avoidance operation is

judged dangerous; an alarm will occur immediately before block 1 and the tool will stop.

Post-compensation intersection of

blocks 1 and 3

Tool center path

Stopped

Programmed path

Block 1

Block 3

Block 2

Fig. 6.6.6.3 (f)

If a pocket in which the bottom is wider than the top, such as that shown in the Fig. 6.6.6.3 (g), is to be

machined, the end-point vector of block 1 and the end-point vector of block 2 are judged to interfere, and

an attempt is made to calculate, as an interference avoidance vector, the intersection vector of the

post-compensation path of block 1 and the post-compensation path of block 3. In this case, the relation

between blocks 1 and 3 is judged an outer one, the post-avoidance path results in overcutting as compared

with the original command. In such a case, interference avoidance operation is judge dangerous; an alarm

will occur immediately before block 1 and the tool will stop.

Stopped

Tool center path

Programmed path

Block 1

Block 3

Block 2

Post-compensation intersection

of blocks 1 and 3

Fig. 6.6.6.3 (g)

If further interference with an interference avoidance vector occurs

If the pocket shown in the Fig. 6.6.6.3 (h) is to be machined, if the number of blocks to read is 3, the

end-point vector of block 1 and the end-point vector of block 2 are judged to interfere, and an attempt is

made to calculate, as an interference avoidance vector, the intersection vector of the post-compensation

path of block 1 and the post-compensation path of block 3. In this case, however, the end-point vector of

block 3 that is to be calculated next further interferes with the previous interference avoidance vector.

- 234 -

B-64484EN-2/02

PROGRAMMING

6.COMPENSATION FUNCTION

If a further interference occurs to the interference avoidance vector once created and output, the

movement in the block will not be performed; an alarm will occur immediately before the block and the

tool will stop.

The intersection vectors of

blocks 3 and 4 further

Tool center path

interfere.

Programmed path

Sropped

Block 5

Block 4

Block 1

Block 3

Block 2

Fig. 6.6.6.3 (h)

NOTE

1 For "If it is judged dangerous to avoid interference" and "If further interference

with an interference avoidance vector occurs", by setting bit 6 (NAA) of

parameter No. 19607 appropriately, it is possible to suppress an alarm to

continue machining. For "If no interference avoidance vector exists", however, it

is not possible to avoid an alarm regardless of the setting of this parameter.

2 If a single block stop occurs during interference avoidance operation, and an

operation is performed which differs from the original movement, such as

manual intervention, MDI intervention, tool radius / tool nose radius

compensation value change, intersection calculation is performed with a new

path. If such an operation is performed, therefore, an interference may occur

again although interference avoidance has been performed once.

- 235 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64484EN-2/02

6.6.7

Tool Radius / Tool Nose Radius Compensation for Input from

MDI

Explanation

MDI operation

During MDI operation, that is, if a program command is specified in MDI mode in the reset state to make

a cycle start, intersection calculation is performed for compensation in the same way as in memory

operation/DNC operation. Compensation is performed in the same way if a subprogram is called from

program memory due to MDI operation.

Subprogram in program memory

MDI command

G90 G00 X0 Y0 ;

O9000 ;

M98 P9000 ;

N1 G41 G17 G91 G01 X10. Y10. D1 ;

M02 ;

N2 Y15. ;

N3 X15. ;

N4 Y-15. ;

N5 X-15. ;

N6 G40 X-10. Y-10. ;

M99 ;

MDI intervention

If MDI intervention is performed, that is, if a single block stop is performed to enter the automatic

operation stop state in the middle of memory operation, DNC operation, and the like, and a program

command is specified in MDI mode to make a cycle start, cutter compensation does not perform

intersection calculation, retaining the last compensation vector before the intervention.

- 236 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64484EN-2/02

6.7

VECTOR RETENTION (G38)

In tool radius / tool nose radius compensation, by specifying G38 in offset mode, it is possible to retain

the compensation vector at the end point of the previous block, without performing intersection

calculation.

Format

(In offset mode)

G38 IP_ ;

IP: Value specified for axial movement

Explanation

Vector retention

By specifying the above command, a vector is created at the end point of the block immediately

preceding the G38 block, vertical to that block. In the G38 block, the vertical vector output in the

previous block is retained. G38 is a one-shot G code. With the next move command without a G38

command, the compensation vector is re-created.

Limitation

Mode

Specify G38 in either G00 or G01 mode. If it is specified in G02 or G03 (circular interpolation) mode, a

radial error may occur at the start and end points.

Start-up/cancel

In start-up/cancel, the operation is as described in Subsections, “Tool Movement in Start-up” and “Tool

Movement in Offset Mode Cancel”. Thus, G38 cannot be specified in the following blocks:

Start-up command (G41 or G42) block

Cancel command (G40) block

Block immediately preceding the cancel command (G40) block

Example

(In offset mode)

(G90)

N1 G38 X10.0 Y0.0 ;

Y axis

N2 G38 X15.0 Y5.0 ;

N3 G38 X10.0 Y0.0 ;

X20.0 ;

X axis

Offset vector

Block N1

Block N2

Tool center path

Program command

(15.0, 5.0)

(10.0, 0.0)

Block N3

- 238 -

B-64484EN-2/02

PROGRAMMING

6.COMPENSATION FUNCTION

6.8

CORNER CIRCULAR INTERPOLATION (G39)

By specifying G39 in offset mode during tool radius / tool nose radius compensation, corner circular

interpolation can be performed. The radius of the corner circular interpolation equals the compensation

value.

Format

In offset mode

G39 ;

I_ J_

G39

I_ K_

;

J_ K_

Explanation

Corner circular interpolation

When the command indicated above is specified, corner circular interpolation in which the radius equals

compensation value can be performed. G41 or G42 preceding the command determines whether the arc is

clockwise or counterclockwise. G39 is a one-shot G code.

G39 without I, J, or K

When G39 is programmed, the arc at the corner is formed so that the vector at the end point of the arc is

perpendicular to the start point of the next block.

G39 with I, J, and K

When G39 is specified with I, J, and K, the arc at the corner is formed so that the vector at the end point

of the arc is perpendicular to the vector defined by the I, J, and K values.

Limitation

Move command

In a block containing G39, no move command can be specified. Otherwise, an alarm will occur.

Inner corner

In an inner corner block, G39 cannot be specified. Otherwise, overcutting will occur.

Corner arc velocity

If a corner arc is specified with G39 in G00 mode, the corner arc block velocity will be that of the F

command previously specified. If G39 is specified in a state in which no F command has never been

specified, the velocity of the corner arc block will be that specified with parameter No. 1411.

- 239 -

B-64484EN-2/02

PROGRAMMING

6.COMPENSATION FUNCTION

6.9

3-DIMENSIONAL TOOL COMPENSATION (G40, G41)

In cutter compensation C, two-dimensional offsetting is performed for a selected plane. In 3-dimensional

tool compensation, the tool can be shifted 3-dimensionally when a 3-dimensional offset direction is

programmed.

Format

Start up (Starting 3-dimensional tool compensation)

When the following command is executed in the cutter compensation cancel mode, the

3-dimensional tool compensation mode is set:

G41 Xp_Yp_Zp_ I_ J_ K_D_ ;

Xp : X-axis or a parallel axis

Yp : Y-axis or a parallel axis

Zp : Z-axis or a parallel axis

I :

J :

See "Explanation".

K :

: Code for specifying as the cutter compensation value (1-3 digits) (D code)

Canceling 3-dimensional tool compensation

When the following command is executed in the 3-dimensional tool compensation

mode, the cutter compensation cancel mode is set:

- When canceling the 3-dimensional tool compensation mode and tool movement at

the same time

G40 Xp_Yp_Zp_ ;

Xp_Yp_Zp_ D00 ;

- When only canceling the vector

G40;

D00;

Selecting offset space

The 3-dimensional space where 3-dimensional tool compensation is to be executed is

determined by the axis addresses specified in the startup block containing the G41

command. If Xp, Yp, or Zp is omitted, the corresponding axis, X-, Y-, or Z-axis (the

basic three axis), is assumed.

(Example)

When the U-axis is parallel to the X-axis, the V-axis is parallel to the Y-axis, and the

W-axis is parallel to the Z-axis

G41 X_I_J_K_D_;

XYZ space

G41 U_V_Z_I_J_K_D_;

UVZ space

G41 W_I_J_K_D_;

XYW space

- 241 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64484EN-2/02

Explanation

3-dimensional tool compensation vector

In 3-dimensional tool compensation mode, the following 3-dimensional tool compensation vector is

generated at the end of each block:

Programmed path

Path after three-dimensional cutter compensation

Three-dimensional cutter compensation

vector

G40

G41

The 3-dimensional tool compensation vector is obtained from the following expressions:

× r

Vx=

(Vector component along the Xp-axis)

× r

Vy=

(Vector component along the Yp-axis)

k × r

Vz=

(Vector component along the Zp-axis)

In the above expressions, i, j, and k are the values specified in addresses I, J, and K in the block. r is the

offset value corresponding to the specified offset number. p is the value obtained from the following

expression:

When the user wants to program the magnitude of a 3-dimensional tool compensation vector as well as its

direction, the value of p in the expressions of Vx, Vy, and Vz can be set as a constant in parameter No.

5011.

If the parameter is set to 0, however, p is determined as follows:

Relationship between 3-dimensional tool compensation and other

compensation functions

Tool length

The specified path is shifted by 3-dimensional tool compensation and the subsequent path

compensation

is shifted by tool length compensation.

When tool offset is specified in the 3-dimensional tool compensation mode, an alarm is

Tool offset

issued (alarm PS0042).

When addresses I, J, and K are all specified at startup, 3-dimensional tool compensation

mode is set. When not all of the addresses are specified, cutter compensation mode is

Cutter compensation

set. Therefore, cutter compensation cannot be specified in 3-dimensional tool

compensation mode and 3-dimensional tool compensation cannot be specified in cutter

compensation mode.

Specifying I, J, and K

Addresses I, J, and K must all be specified to start 3-dimensional tool compensation. When even one of

the three addresses is omitted, two-dimensional cutter compensation is activated. When a block specified

in 3-dimensional tool compensation mode contains none of addresses I, J, and K, the same vector as the

vector generated in the previous block is generated at the end of the block.

G42

Generally, G41 is specified to start 3-dimensional tool compensation. Instead of G41, G42 can be

specified for startup. With G42, 3-dimensional tool compensation is performed in the opposite direction.

- 242 -

B-64484EN-2/02

PROGRAMMING

6.COMPENSATION FUNCTION

Offset vector in interpolation

When circular interpolation, helical interpolation

(both specified with G02, G03), or involute

interpolation (G02.2, G03.2) is specified, the vector generated in the previous block is maintained.

Vector generated in the block before an arc

The same vector is

generated.

Programmed path

Path after three-dimensional cutter

compensation

Three-dimensional cutter compensation vector

Reference position return check (G27)

Before specifying reference position return check (G27), cancel 3-dimensional tool compensation. In the

compensation mode, G27 brings the tool to a position shifted by the offset value. If the position the tool

reached is not the reference position, the reference position return LED does not go on (the alarm PS0092

alarm is issued).

Return to a reference position (G28, G30, G30.1)

When return to the reference position (G28), to the second, third, or fourth reference position (G30), or to

the floating reference position (G30.1) is specified, the vector is cleared at a middle point.

Alarm issued at startup

If one of the following conditions is present at the startup of 3-dimensional tool compensation, an alarm is

issued:

• Two or more axes are specified in the same direction. (alarm PS0047)

• Although Xp, Yp, or Zp is omitted, the basic three axes are not set. (alarm PS0048)

Alarm during 3-dimensional tool compensation

If one of the following G codes is specified in the 3-dimensional tool compensation mode, an alarm is

issued:

G05 High-speed cycle machining (alarm PS0178)

G31 Skip function (alarm PS0036)

G51 Scaling (alarm PS0141)

Commands that clear the vector

When one of the following G codes is specified in 3-dimensional tool compensation mode, the vector is

cleared:

G73 Peck drilling cycle

G74 Reverse tapping cycle

G76 Fine boring

G80 Canned cycle cancel

G81 Drilling cycle, spot boring

G82 Drilling cycle, counter boring

G83 Peck drilling cycle

G84 Tapping cycle

G85 Boring cycle

G86 Boring cycle

G87 Back boring cycle

G88 Boring cycle

G89 Boring cycle

G53 Machine coordinate system selection

- 243 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64484EN-2/02

Commands that generate the same vector as the vector in the previous block

When one of the following G codes is specified in 3-dimensional tool compensation mode, the same

vector as the vector generated in the previous block is generated at the end point of the next movement:

G02 Circular or helical interpolation (CW)

G03 Circular or helical interpolation (CCW)

G02.2 Involute interpolation (CW)

G03.2 Involute interpolation (CCW)

G04 Dwell

G10 Data setting

G22 Stored stroke check function enabled

6.10 TOOL COMPENSATION VALUES, NUMBER OF

COMPENSATION VALUES, AND ENTERING VALUES

FROM THE PROGRAM (G10)

Tool compensation values include tool geometry compensation values and tool wear compensation (Fig.

6.10 (a)).

Reference

position

OFS_G

OFS_W

OFS_G

: Geometry compensation value

OFS_W

: Wear compensation value

Fig. 6.10 (a) Geometric compensation and wear compensation

Tool compensation values can be entered into CNC memory from the MDI panel (see section III-11.1.1)

or from a program.

A tool compensation value is selected from the CNC memory when the corresponding code is specified

after address H or D in a program.

The value is used for tool length compensation, cutter compensation, or the tool offset.

Three types of tool compensation memories are available according to the compensation value

configuration: tool compensation memory A, B, and C. One of the types can be selected.

Explanation

Tool compensation memory A

In tool compensation memory A, memory for geometry compensation and memory for wear

compensation are not distinguished from each other. So, the sum of geometry compensation and wear

compensation values is to be set in the compensation memory. Moreover, no distinction is made between

memory for cutter compensation (for D code) and memory for tool length compensation (for H code).

Setting example

Compensation number

Compensation value (geometry+wear)

Common to D code/H code

001

10.000

For D code

002

20.000

For D code

003

100.000

For H code

- 244 -

B-64484EN-2/02

PROGRAMMING

6.COMPENSATION FUNCTION

Tool compensation memory B

In tool compensation memory B, memory for geometry compensation and memory for wear

compensation are prepared separately. So, geometry compensation values and wear compensation values

can be set separately. However, no distinction is made between memory for cutter compensation (for D

code) and memory for tool length compensation (for H code).

Setting example

Common to D code/H

Compensation number

For geometry compensation

For wear compensation

code

001

10.100

0.100

For D code

002

20.200

0.200

For D code

003

100.000

0.100

For H code

Tool compensation memory C

In tool compensation memory C, memory for geometry compensation and memory for wear

compensation are prepared separately. So, geometry compensation values and wear compensation values

can be set separately. Moreover, memory for cutter compensation (for D code) and memory for tool

length compensation (for H code) are prepared separately.

Setting example

D code

H code

Compensation

For geometry

For wear

For geometry

For wear

number

compensation

001

10.000

0.100

100.000

0.100

002

20.000

0.200

200.000

0.300

In addition, if the cutting point command option is enabled, additional memory for corner R offset (for D

code) is prepared separately.

Setting example

D code

H code

Compensation

(For tool compensation)

(For corner R offset)

number

For geometry

For wear

For geometry

For wear

For geometry

For wear

compensation

001

10.000

0.100

1.000

0.100

100.000

0.100

002

20.000

0.200

2.000

0.400

200.000

0.300

Unit and valid range of tool compensation values

A unit and valid range of tool offset values can be selected from the following by parameter setting:

Unit and valid range of tool compensation values (metric input)

OFE

OFD

OFC

OFA

Unit

Valid range

0.01mm

±9999.99mm

0.001mm

±9999.999mm

0.0001mm

±9999.9999mm

0.00001mm

±9999.99999mm

0.000001mm

±999.999999mm

Unit and valid range of tool compensation values (inch input)

OFE

OFD

OFC

OFA

Unit

Valid range

0.001inch

±999.999inch

- 245 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64484EN-2/02

OFE

OFD

OFC

OFA

Unit

Valid range

0.0001inch

±999.9999inch

0.00001inch

±999.99999inch

0.000001inch

±999.999999inch

0.0000001inch

±99.9999999inch

Number of tool compensation data items

The number of tool compensation data items used by the entire system varies from one machine to

another. Refer to the relevant manual of the machine tool builder.

Format

The format for programming depends on the type of tool compensation memory.

For tool compensation memory A

G10 L11 P_ R_ Q_ ;

Tool compensation number

Tool compensation value

Imaginary tool nose number

For tool compensation memory B

G10 L_ P_ R_ Q_ ;

: Type of compensation memory

L10 : Geometry compensation value

L11 : Wear compensation value

: Tool compensation number

R_ : Tool compensation value

Q_ : Imaginary tool nose number

For tool compensation memory C

G10 L_ P_ R_ Q_ ;

: Type of compensation memory

L10 : Geometry compensation value corresponding to an H code

L11 : Wear compensation value corresponding to an H code

L12 : Geometry compensation value corresponding to a D code

L13 : Wear compensation corresponding to a D code

L110 : Geometry compensation value corresponding to a D code (for corner R

offset)

L111 : Wear compensation corresponding to a D code (for corner R offset)

: Tool compensation number

R_ : Tool compensation value

Q_ : Imaginary tool nose number

By specifying G10, a tool compensation value can be set or modified.

When G10 is specified by absolute input (G90), the specified value is used as the new tool compensation

value.

When incremental input (G91) is used, a specified value added to the tool compensation value currently

set is used as the new tool compensation value.

- 246 -

B-64484EN-2/02

PROGRAMMING

6.COMPENSATION FUNCTION

NOTE

1 Address R follows the increment system for tool offset values.

2 If L is omitted for compatibility with the conventional CNC format, or L1 is

specified, the same operation as when L11 is specified is performed.

3 Set a imaginary tool nose number when the cutter compensation function is

specified and a imaginary tool nose direction is used.

6.11 COORDINATE SYSTEM ROTATION (G68, G69)

A programmed shape can be rotated. By using this function it becomes possible, for example, to modify a

program using a rotation command when a workpiece has been placed with some angle rotated from the

programmed position on the machine. Further, when there is a pattern comprising some identical shapes

in the positions rotated from a shape, the time required for programming and the length of the program

can be reduced by preparing a subprogram of the shape and calling it after rotation.

Angle of rotation

Center of rotation

Fig. 6.11 (a) Coordinate system rotation

Format

⎧G17

⎫

⎪

G18

Start rotation of a coordinate system.

⎨

⎬G68 α_β_ R_ ;

⎪

G19

⎩

⎭

Coordinate system rotation mode

(The coordinate system is rotated.)

G69 ;

Coordinate system rotation cancel command

G17 (G18 or G19) : Select the plane in which contains the figure to be rotated.

α_β_ : Absolute programming for two of the X_, Y_, and Z_ axes that correspond to the

current plane selected by a command (G17, G18, or G19). The command

specifies the coordinates of the center of rotation for the values specified

subsequent to G68

: Angular displacement with a positive value indicates counter clockwise rotation.

Bit 0 (RIN) of parameter No. 5400 selects whether the specified angular

displacement is always considered an absolute value or is considered an

absolute or incremental value depending on the specified G code (G90 or G91).

Least input increment

0.001 deg

Valid data range

-360,000 to 360,000

- 247 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64484EN-2/02

Angle of rotation R (incremental value)

Center of

Angle of rotation (absolute value)

rotation

(α, β)

Fig. 6.11 (b) Coordinate system rotation

NOTE

When a decimal fraction is used to specify angular displacement (R_), the 1's

digit corresponds to degree units.

Explanation

G code for selecting a plane: G17,G18 or G19

The G code for selecting a plane (G17,G18,or G19) can be specified before the block containing the G

code for coordinate system rotation (G68). G17, G18 or G19 must not be designated in the mode of

coordinate system rotation.

Incremental programming in coordinate system rotation mode

The center of rotation for an incremental programming programmed after G68 but before an absolute

programming is the tool position when G68 was programmed (Fig. 6.11 (c)).

Center of rotation

When α_β_ is not programmed, the tool position when G68 was programmed is assumed as the center of

rotation.

Angular displacement

When R_ is not specified, the value specified in parameter No. 5410 is assumed as the angular

displacement.

To specify angular displacement (R_) in 0.00001 degrees (one hundred-thousandth), set bit 0 (FRD) of

parameter No. 11630 to 1. In this case, angular displacement R is specified within the range of -36000000

to 36000000.

Coordinate system rotation cancel command

The G code used to cancel coordinate system rotation (G69) may be specified in a block in which another

command is specified.

Tool compensation

Tool radius/tool nose radius compensation, tool length compensation, tool offset, and other compensation

operations are executed after the coordinate system is rotated.

Relationship with 3-dimensional coordinate conversion (G68, G69)

Both coordinate system rotation and 3-dimensional coordinate conversion use the same G codes: G68 and

G69. The G code with I, J, and K is processed as a command for 3-dimensional coordinate conversion.

The G code without I, J, and K is processed as a command for two-dimensional coordinate system

rotation.

- 248 -

B-64484EN-2/02

PROGRAMMING

6.COMPENSATION FUNCTION

Limitation

Commands related to reference position return and the coordinate system

In coordinate system rotation mode, G codes related to reference position return (G27, G28, G29, G30,

etc.) and those for changing the coordinate system (G52 to G59, G92, etc.) must not be specified. If any

of these G codes is necessary, specify it only after canceling coordinate system rotation mode.

Incremental programming

The first move command after the coordinate system rotation cancel command (G69) must be specified

with absolute values. If an incremental move command is specified, correct movement will not be

performed.

Note on the specification of one axis in coordinate system rotation

With the parameter below, a move position in the case where one axis is specified in the absolute mode

can selected. If two axes are specified, a movement is made to the same position, regardless of the setting

of the parameter.

Bit 5 (AX1) of parameter No. 11600

If one axis is specified in the absolute mode when the coordinate system rotation mode is set:

0: The specified position is first calculated in the coordinate system before rotation then the

coordinate system is rotated.

1: The coordinate system is first rotated then a movement is made to the specified position in the

rotated coordinate system. (FS16i/18i/21i-compatible specification)

This parameter changes the handling of coordinates on axes not specified, so that a position to be

reached by movement changes.

(Example)

G90 G0 X0 Y0

G01 X10. Y10. F6000

G68 X0 Y0 R45

Specifies coordinate system rotation.

Y14.142

Specifies one axis

(1)

G69

When bit 5 (AX1) of parameter No. 11600= 0:

The specified position is calculated in the coordinate system (XY) before rotation then the

coordinate system is rotated. So, with the specification of (1), the position on the unspecified X

axis is X10, and the specified position is (X10,Y14.142). Next, a movement is made to the

move position (X-2.929,Y17.071) obtained by 45° rotation.

Move position

: X-2.929,Y17.071

Specified position

: X10,Y14.142

Coordinates before

Tool path

45°

coordinate system rotation is

specified

: X10,Y10

- 249 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64484EN-2/02

When bit 5 (AX1) of parameter No. 11600= 1:

With the specification of (1), coordinates (X10,Y10) before coordinate system rotation are

converted to coordinates (X'14.142,Y'0) in the coordinate system (X'Y') obtained by 45°

rotation. Next, a movement is made to the specified position (X'14.142,Y'14.142), that is, the

move position (X0,Y20).

Specified position

: X'14.142,Y'14.142

Move position

: X0,Y20

Tool path

Coordinates before coordinate

system rotation is specified

: X10,Y10

Conversion

Coordinates in rotated coordinate

system

45°

: X'14.142,Y'0

Explanation

Absolute/Incremental position commands

N1 G92 X-500.0 Y-500.0 G69 G17 ;

N2 G68 X700.0 Y300.0 R60.0 ;

N3 G90 G01 X0 Y0 F200 ;

(G91X500.0Y500.0)

N4 G91 X1000.0 ;

N5 G02 Y1000.0 R1000.0 ;

N6 G03 X-1000.0 I-500.0 J-500.0 ;

N7 G01 Y-1000.0 ;

N8 G69 G90 X-500.0 Y-500.0 M02 ;

Tool path when the incremental

command is designated in the N3

block (in parenthesis)

Originally programmed tool path

Center of rotation

(700.0,300.0)

(0,0)

60º

(-500.0,-500.0)

Tool path after rotation

Fig. 6.11 (c) Absolute/incremental programming during coordinate system rotation

- 250 -

B-64484EN-2/02

PROGRAMMING

6.COMPENSATION FUNCTION

Cutter compensation and coordinate system rotation

It is possible to specify G68 and G69 in cutter compensation mode.

The rotation plane must coincide with the plane of cutter compensation.

N1 G92 X0 Y0 G69 G01 ;

N2 G42 G90 X1000 Y1000 F1000 D01 ;

N3 G68 R-30000 ;

N4 G91 X2000 ;

N5 G03 Y1000 R1000 J500 ;

N6 G01 X-2000 ;

N7 Y-1000 ;

N8 G69 G40 G90 X0 Y0 M30 ;

Programmed shape before

coordinate system rotation

Programmed shape

after coordinate

system rotation

30q

(0, 0)

Tool path

Fig. 6.11 (d) Cutter compensation and coordinate system rotation

Scaling and coordinate system rotation

If a coordinate system rotation command is executed in the scaling mode (G51 mode), the coordinate

value (a, b) of the rotation center will also be scaled, but not the rotation angle (R). When a move

command is issued, the scaling is applied first and then the coordinates are rotated.

A coordinate system rotation command (G68) should not be issued in cutter compensation mode (G41,

G42) on scaling mode (G51). The coordinate system rotation command should always be specified prior

to setting the cutter compensation mode.

When the system is not in cutter compensation mode, specify the commands in the following order :

G51 ;

Scaling mode start

G68 ;

Coordinate system rotation mode start

G69 ;

Coordinate system rotation mode cancel

G50 ;

Scaling mode cancel

When the system is in cutter compensation, specify the commands in the following order (Fig. 6.11

(e)) :

(cutter compensation cancel)

G51 ;

Scaling mode start

G68 ;

Coordinate system rotation start

G41 ;

Cutter compensation mode start

- 251 -

B-64484EN-2/02

PROGRAMMING

6.COMPENSATION FUNCTION

Repetitive commands for coordinate system rotation

It is possible to store one program as a subprogram and recall subprogram by changing the angle.

Sample program for when parameter RIN (No. 5400#0) is set to 1.

The specified angular displancement is treated as an absolute or

incremental value depending on the specified G code (G90 or G91).

G92 X0 Y0 G69 G17;

G01 F200 H01 ;

M98 P2100 ;

M98 P072200 ;

G00 G90 X0 Y0 M30 ;

O 2200 G68 X0 Y0 G91 R45.0 ;

G90 M98 P2100 ;

M99 ;

O 2100 G90 G01 G42 X0 Y-10.0 ;

X4.142 ;

X7.071 Y-7.071 ;

G40 ;

M99 ;

Programmed path

(0, 0)

When offset is

applied

(0, -10.0)

Subprogram

Fig. 6.11 (f) Coordinate system rotation command

- 253 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64484EN-2/02

6.12 GRINDING WHEEL WEAR COMPENSATION

A compensation vector is created on an extension of the line from a specified point (compensation center)

to a specified end point position on a specified compensation plane.

Compensation vector

Programmed path

Compensation center

Tool center path

Fig. 6.12 (a)

Format

Compensation center selection

G41 P_(n=1,2,3);

G41P1: First compensation center selection Coordinates

(parameters Nos. 5081 and 5082))

G41P2: Second compensation center selection Coordinates

(parameters Nos. 5083 and 5084))

G41P3: Third compensation center selection Coordinates

(parameters Nos. 5085 and 5086))

Start-up

D_; non-zero D code

Compensation mode cancel

D0;

Compensation vector retention

G40;

Explanation

Compensation center setting and selection

There can be three compensation centers, and the coordinates of the centers can be set with parameters

Nos. 5081 to 5086.

Which of these three centers to use can be determined with G41Pn (where n = 1, 2, or 3).

G41 P1 ;

First compensation center selection

G41 P2 ;

Second compensation center selection

G41 P3 ;

Third compensation center selection

When selecting a compensation center, be sure to specify P1, P2, or P3 at the same time.

If no P is specified or if a value other than

1 to

3 is specified, alarm PS

1618,

“ILLEGAL

P-DATA(WHEEL WEAR COMPENSATION)” is issued.

The coordinates of the compensation centers (parameters Nos. 5081 to 5086) must be set as those in the

workpiece coordinate system.

- 254 -

B-64484EN-2/02

PROGRAMMING

6.COMPENSATION FUNCTION

Start-up

By specifying a compensation center and specifying a non-zero D code, the system enters compensation

mode.

Even if the block in which the D code is specified does not contain a move command, a compensation

vector is created and movement is performed.

Compensation vector

A compensation vector is created on an extension of the line from the compensation center to a specified

end point position, the length of the vector being equal to the offset value specified with its offset number

with a D code. (See Fig. 6.12 (a).)

If the offset value is positive, the compensation vector is added to the specified end point position, and if

the offset value is negative, the compensation vector is subtracted from the specified end point position.

＋

Compensation vector (＋)

Compensation

Programmed path

center

Tool center path

Y＋

Fig. 6.12 (b) Offset value (+)

Compensation vector (-)

＋

Programmed path

Compensation

center

Tool center path

Y＋

Fig. 6.12 (c) Offset value (-)

Compensation mode cancel

Specifying D0 causes the compensation mode to be canceled, so that the compensation vector is not

created.

Compensation vector retention

By specifying G40, it is possible to place the system in a mode in which the created compensation vector

is retained. Until the system enters the next new compensation mode, the specified end point position is

shifted by the vector.

If D0 is specified in the compensation vector retention mode, the retained vector is cleared and the

compensation mode is canceled.

Circular and helical interpolation

This compensation is also effective to circular interpolation. If the radius at the start point of the arc

differs from the radius at the end point, the arc cannot be a correct one. It will be a spiral one.

This is also true of helical interpolation.

- 255 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64484EN-2/02

Compensation vector

Arc center

Tool center path

Programmed path

Compensation center

Fig. 6.12 (d)

A check of the arc radius error limit (parameter No. 3410) is performed even on the value after

compensation.

Circular interpolation in G40 mode

Executing a G40 mode arc command causes the arc center to be shifted by the vector. This makes an arc,

not a spiral.

Programmed arc center

Retained vector

Tool center path

Programmed path

Fig. 6.12 (e)

Exponential interpolation

This compensation is also effective to exponential interpolation. Exponential interpolation is performed

on the position after compensation is applied.

Compensation plane and plane selection with G17/G18/G19

In the compensation mode (and in the compensation vector retention mode), a compensation vector is

constantly created for the axes on the compensation plane determined with a parameter. Creation of a

compensation vector is not related to the plane selection with G17/G18/G19.

It is possible to apply compensation on a compensation plane (for example, the YZ plane) while

performing circular interpolation on the XY (G17) plane.

If, in the compensation mode, a move command is issued for one compensation axis, and the

compensation vector components on the other axis are changed due to the creation of a compensation

vector, movement along this axis is performed.

- 256 -

B-64484EN-2/02

PROGRAMMING

6.COMPENSATION FUNCTION

(Example 1)

The compensation axes are set as the Y- and Z-axes, and a linear interpolation command is executed

on the X- and Y-axes.

Programmed path a → b

Path after compensation a’ → b’

V_ay

V_by

Fig. 6.12 (f) Path on the X-Y plane

V_ay

V_a

V_az

V_by

V_b

V_bz

Compensation center

V_by

Fig. 6.12 (g) Path on the Y-Z plane

(Example 2)

The compensation axes are set as the Y- and Z-axes, and a circular interpolation

command is

executed on the X- and Y-axes.

Programmed path a → b

Path after compensation a’ → b’

Arc center

Fig. 6.12 (h) Path on the X-Y plane

- 257 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64484EN-2/02

V_ay

V_a

V_az

V_by

V_b

Vbz

Compensation center

V_by

Fig. 6.12 (i) Path on the Y-Z plane

Compensation cancel mode

Immediately after the power is turned on and after a reset, the system is in the compensation cancel mode.

Changing the coordinate system

To change the coordinate system, cancel the compensation mode first.

Return to the reference position (G28, G30)

To specify a return to the reference position (G28, G30), cancel the compensation mode.

Limitation

Relations with the coordinate conversion function

Functions such as programmable mirror image, scaling, and coordinate system rotation cannot be applied

to the coordinates of the compensation center.

Relations with other offset functions

In a system with this compensation attached, cutter compensation and 3-dimensional tool compensation

cannot be used. This compensation can be used simultaneously as tool length offset and tool offset.

Changing the compensation axis

To change the compensation axis, enter the compensation cancel mode.

- 258 -

B-64484EN-2/02

PROGRAMMING

6.COMPENSATION FUNCTION

6.13 ACTIVE OFFSET VALUE CHANGE FUNCTION BASED ON

MANUAL FEED

Overview

When rough machining/semifinish machining is to be performed using a single tool, you may make a fine

adjustment of a tool length compensation value or cutter compensation value. Moreover, at setup time,

you may want to make a fine adjustment of a workpiece origin offset once set. With this function, a travel

distance moved on an axis by manual feed is automatically added to the workpiece coordinate system or

the currently valid offset number among the specified offset values (tool length compensation value/cutter

compensation value/workpiece origin offset) to make a offset value change.

Explanation

Active offset value change mode

The active offset value change mode is set using the active offset value change mode signal. In this mode,

a travel distance moved on an axis by manual feed is automatically added to the workpiece coordinate

system or the currently valid offset number among the specified offset values (tool length compensation

value/cutter compensation value/workpiece origin offset). The types of manual feed usable to make an

offset value change in this mode are manual handle feed, incremental feed, and jog feed.

CAUTION

1 When a movement is being made on an axis for which an offset value is to be

changed, do not set the active offset value change mode.

2 In the active offset value change mode, do not reset the relative coordinate to 0

or preset the relative coordinate to a specified value.

Specifying an offset value to be changed

The active offset selection signal is used to specify one of three types of offset values: tool length

compensation value, cutter compensation value, and workpiece origin offset. In the active offset value

change mode, an offset value selected is indicated by blinking display in the state display area on the

screen as follows:

Offset value selected

State display

Tool length compensation value

LEN

Cutter compensation value

RAD

Workpiece origin offset

WZR

CAUTION

When a movement is being made on an axis for which an offset value is to be

changed in the active offset value change mode, do not change the specification

of the offset value to be changed.

Changing a tool length compensation value

The tool length compensation value with the offset number corresponding to an H code specified in

automatic operation is changed. If there is no currently valid tool length compensation value as in a case

where no H code is specified after a cycle start, no tool length compensation value change is made even

when a movement is made on an axis by manual feed.

With a movement on a linear axis, a tool length compensation value change can be made. With a

movement on a rotation axis, no tool length compensation value change can be made. While a tool length

compensation value is being changed, a movement by manual feed can be made on one axis only.

- 259 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64484EN-2/02

Example

- Specified H code: H10

- Value set with offset number 10: 54.700 mm

- Travel distance on the Z-axis by manual feed: -2.583 mm

In this example, the value of offset number 10 becomes:

54.700 + (-2.583) = 52.117 mm

CAUTION

A tool length compensation value can be changed by a movement on any linear

axis. When an offset value change for an axis is undesirable, interlock the axis.

NOTE

A changed tool length compensation value is handled according to bit 6 (EVO) of

parameter No. 5001 and bit 6 (AON) of parameter No. 5041.

Changing a cutter compensation value

The cutter compensation value with the offset number corresponding to a D code specified in automatic

operation is changed. If there is no currently valid cutter compensation value as in a case where no D

code is specified after a cycle start, no cutter compensation value change is made even when a movement

is made on an axis by manual feed.

With a movement on a linear axis, a cutter compensation value change can be made. With a movement on

a rotation axis, no cutter compensation value change can be made. While a cutter compensation value is

being changed, a movement by manual feed can be made on one axis only.

When operation is stopped in the cutter compensation mode to make a cutter compensation value change,

a movable travel distance on one axis is added, regardless of the direction of the compensation vector at

stop time.

Example

- Specified D code: H15

- Value set with offset number 15: 6.500mm

- Travel distance on the X-axis by manual feed: 2.379mm

- Travel distance on the Y-axis by manual feed: -0.572mm

In this example, the value of offset number 15 becomes:

6.500+2.379+(-0.572)= 8.307mm

CAUTION

A cutter compensation value can be changed by a movement on any linear axis.

When an offset value change for an axis is undesirable, interlock the axis.

NOTE

A changed cutter compensation value is handled according to bit 4 (EVR) of

parameter No. 5001.

Changing a workpiece origin offset value

The workpiece origin offset of the workpiece coordinate system corresponding to a G code from G54 to

G59 or from G54.1 P1 to P48 (300) specified during automatic operation is changed on an axis-by-axis

basis. A valid workpiece coordinate system exists at all times. So, when a movement is made on an axis

by manual feed, the workpiece origin offset of the workpiece coordinate system is changed without fail.

This change can be made by a movement on an arbitrary axis, which may be a linear axis or a rotation

axis. While a workpiece origin offset change is being made, movements can be made on multiple axes by

manual feed.

- 260 -

B-64484EN-2/02

PROGRAMMING

6.COMPENSATION FUNCTION

Example

- Specified workpiece coordinate system : G56

- Workpiece origin offset of G56 (X axis) : 50.000

- Workpiece origin offset of G56 (Y axis) : -60.000

- Workpiece origin offset of G56 (Z axis) : 5.000

- Workpiece origin offset of G56 (A axis) : 5.000

- Workpiece origin offset of G56 (B axis) : 15.000

- Travel distance on the X axis by manual feed : -10.000mm

- Travel distance on the Y axis by manual feed : -5.000mm

- Travel distance on the Z axis by manual feed : 10.000mm

- Travel distance on the A axis by manual feed : 8.000mm

- Travel distance on the B axis by manual feed : -2.000mm

In this example, the workpiece origin offsets of G56 are as follows:

- X axis : 50.000+(-10.000) = 40.000

- Y axis : -60.000+(-5.000) = -65.000

- Z axis : 5.000+10.000 = 15.000

- A axis : 5.000+8.000 = 13.000

- B axis : 15.000+(-2.000) = 13.000

Operation depending on each tool offset memory

Offset value change operation varies according to tool offset memory A/B/C as follows:

Tool offset

Changed offset value

memory

No distinction is made between a tool length compensation value and cutter compensation value.

The value specified with the offset number corresponding to the currently valid H code or D code is

changed.

No distinction is made between a tool length compensation value and cutter compensation value.

The value specified with the offset number corresponding to the currently valid H code or D code is

changed.

Depending on the setting of bit 4 (ASG) of parameter No. 5000, a geometry compensation value or

wear compensation value is changed.

The tool length compensation value and cutter compensation value specified with the offset numbers

corresponding to the currently valid H code and D code are changed.

Depending on the setting of bit 4 (ASG) of parameter No. 5000, a geometry compensation value or

wear compensation value is changed.

Presetting the relative position indication

By setting bit 5 (APL) of parameter No. 3115 to 1, the relative position indication (counter) can be

automatically preset to 0 when the active offset value change mode is selected. In this case, the changed

offset value can be restored to the original value by returning the relative position indication (counter) to

0 by manual feed.

Emergency stop, servo alarm

If an emergency stop occurs, a servo alarm is issued, or servo excitation is turned off, an offset value

change is made also for a travel distance on an axis moved by follow-up in the active offset value change

mode.

NOTE

If a tool length compensation value or cutter compensation value is selected as

an offset value to be changed, no offset value change is made for a travel

distance on a rotation axis moved by follow-up.

- 261 -

FANUC Series 30i-MODEL B, 31i-MODEL B, 32i-MODEL B. For Machining Center System. OPERATOR'S MANUAL - page 9